The vast majority of engineered products have multiple components that need to fit together.
Sometimes you need components to slip together easily, while other times, you need components
to press together and not come apart. There’s a systematic way to design parts so they fit
together exactly the way you want on the first try, every time, and in this video, we’re
going to show you how. The engineering term for this consideration is “fits and tolerances”.
Let’s define these terms. Most of the time, especially in CAD, we just type single, exact
numbers into the computer for our dimensions. That’s called a “nominal” dimension.
But when it comes time to actually make that part, we won’t be able to manufacture the
features to exactly those dimensions. Each feature might be slightly larger or smaller
than the number we originally typed into the computer. So, we need to specify a “tolerance”
which tells the person manufacturing the part how much of a variation from our nominal dimension
is acceptable. Different manufacturing processes are capable of different tolerances. This
chart shows a variety of different manufacturing processes, as well as a general idea of the
tolerance that can be expected. It’s important to remember that tolerance capability corresponds
to a large production run, where factors like tool and machine wear, deflection, sharpening,
and the natural variation of different processes apply. A very common mistake that new engineers
make is selecting tolerances that are far tighter than necessary. As the tolerances
become tighter, the cost to manufacture the part grows exponentially. So how tight of
a tolerance do you need? Tolerances typically come into play when designing fits. In some
cases, you might want components to slip easily together, but not have a lot of perceptible
play. In other cases, lots of relative movement is okay. You might even need to have two components
come together permanently and not come apart. These different cases are called “fits”.
Machinery’s Handbook is the go-to reference for designing fits. Fits have a particular
naming convention of a two-letter abbreviation followed by a number. The letters denote the
type of fit, and the number corresponds to the tolerance class of the fit, with larger
numbers representing looser tolerances. This graph shows all the standard ASME fits. The
solid bars represent the acceptable tolerance of the shaft, while the hashed bars represent
the acceptable tolerance of the hole. The scale of this graph corresponds to a one-inch
nominal shaft. This video deals primarily with ASME fits in the inch system, but there
is a similar convention for metric. The naming convention is different, but the general concept
is the same. For more information, you can reference Machinery’s handbook, or ISO 286-2.
Since the chart only applies for a one-inch basic size, we need to use tables to design
for other sizes. The process is easy, and we’ll show you how with an example. The
first fit we’ll show you is the loosest. This is a LC11, and you can see there’s
lots of clearance. To design this fit, first we’ll look up the LC11 column. Then, we’ll
find the row that corresponds to our basic size. At the intersection of the size and
fit, we have a tolerance range for both the shaft and hole. Note that these numbers are
in thousandths of an inch. You’ll use this same procedure to design all the other fits
that we’ll talk about. These tolerances are extremely loose, so drilling the hole
with a regular drill is sufficient. Hitting the shaft tolerance on the lathe is also no
problem, and other processes like forming and extrusion will probably hit it as well.
This fit is used where you don’t need accurate alignment of the mating features. The clearance
around a bolt is a good example of this, since you typically don’t use a bolt for precision
alignment. This is a slightly tighter locational fit, LC9. It provides less clearance and has
a tighter tolerance than the LC11. This is probably about the tightest hole tolerance
that can be drilled, but turning shouldn't be a problem for the shaft tolerance. You
can see that the LC9 fit is a bit tighter than the LC11, but both can still be easily
achieved with standard equipment and tooling. The next category of fits is called “running”
fits. A running fit is typically used when you need two parts to mate together freely,
or that’s to say, without any force, but you need some degree of precision in their
alignment. We reamed this RC6 hole, but you can probably achieve this tolerance on a CNC
mill if you compensate for tool diameter in the control. A drill is not likely to hit
this tolerance every time. Depending on the size, this is probably about the tightest
shaft tolerance that you can expect to hit consistently by turning. This is the fit to
use when you need two parts to align to each other, but some clearance is acceptable. This
is the tightest fit that can be readily achieved with normal manufacturing processes, and without
undue effort. For the rest of the fits in this video, we’re going to have to work
a bit to hit the tolerances, and you’re going to want to be absolutely sure you need
this in your design, because you’ll be paying for that care and attention. This is an RC3
fit, which is a tighter running fit. In general, this fit is going to have almost no perceptible
play. This hole will need to be reamed or bored. You can also interpolate it on a CNC
mill, but you will probably have to update the wear offsets throughout the production
run to compensate for tool wear, and you will need to be sure that tool deflection isn’t
causing the feature to taper with depth. A dialed-in and rigid lathe setup might be able
to hit this shaft tolerance consistently, but as with the hole, you will need to perform
regular inspections throughout and adjust the wear offsets. A lot of parts, especially
flexible ones or those made of tough materials, will require grinding. Here is a comparison
of the two running fits. The RC6 has some perceptible play, while the RC3 has almost
none. RC3 and tighter will precisely align components but can still be assembled easily
by hand. This next type of fit is called a “transition fit” and it requires a slight
amount of force to assemble and disassemble. However, there is absolutely no play once
the pieces are assembled. The tolerances required for the LT3 fit are about the same as for
the RC3, but the range of the shaft has been shifted so that there is a slight amount of
interference. If we add a bit more interference, we create what’s called a “force fit”
or “press fit.” These fits usually require a press to assemble, and are intended to be
a permeant connection. We hope you enjoyed this video. If you have other topics in mechanical
design engineering that you'd like to learn about, leave a comment and let us know. We're
coming out with new videos soon, so please be sure to subscribe. Thanks!